How does the drawings module still suck so bad?

[yoshimitsuspeed]

Half the time you try to place a dimention it pops up with the warning then you have to reassociate it to get rid of the warning.
Make one change in the modle and every single dimension looses it's association and you have to go through and reassociate all of them. Oftentimes that won't even work so you have to delete all your dimensions and annotations and redo them all.
I mean seriously? We won't even get into all the features, capability and workflow improvement that is lacking.

Please please fix these things.

[yoshimitsuspeed]

You can dimension by selecting two lines however if you need to reassociate that dimension it will only select points, not the lines. If the points are not alinged it will not give you the proper dimension.

Centerline should have more capabilities. For example you don't always have to faces to select. If say you are dimensioning a thread or tapered wall. You should be able to select a cross line at the top or bottom of the hole and be able to make the centerline perpendicular to that line.
Or you should have other means of defining centerlines.

[Anonymous]

Hi @yoshimitsuspeed,

I occasionally have problems with associations, but not as bad as you seem to. I agree, sometimes it can be strange to find a dimension didn't associate correctly.

I very rarely have an entire model lose it's association though. Only when I make a radical change (like splitting the part or something that changes the feature completely). Really, this just means I have to have my model "complete" before I begin the drawing.

When, exactly, do models lose their dimensional associativity for you? if you give some more details about your workflow, I can give you some tips. But unless I know exactly what is wrong, I can't even give suggestions (and it is hard to fix something if you don't know what is broken).

As for workflow issues, the only thing I find lacking is hotkeys (there are none in the drawing workspace). Once again, unless you are detailed, no one can fix anything or give suggestions.

For the ease of the users giving suggestions (and the staff) perhaps write it up like this:

Expected workflow

Step 1

Step 2

Etc

Actual Workflow

Step 1

Step 2

etc

And include what goes wrong when, for example, "Whenever I use "split body" on my model, it cases all drawing dimensions to lose association" so they can work on reproducing and fixing it. Just saying "Please fix things" doesn't give anyone any idea of what is wrong, what causes it to go wrong, and how you expect it to act.

Thank you, and I look forward to seeing your response.

[yoshimitsuspeed]

I just gave many specifics.
More importantly many people who have a lot more patience and take the time to give much more detail do so all the time. We have been for years.

For associations loosing dimension. In this case today I was dimensioning a piston. The first time I rolled the model back to when the piston wasn't visible and then accidentally refreshed the drawing before rolling forward again. Naturally the whole drawing turns into a clusterf. So I roll back, put the model back to where it should be in the timeline and then save and refresh the drawing. I wasn't at all surprised to see all dimensions lost their association. I wasn't surprised but I still find this completely unacceptable. If it really throws F360 off this much then it should have a popup or something asking if you really want to refresh or make changes first. If more than one or two drawings are about to loose association this should happen.
After this nothing would reassociate so I had to redimension the whole drawing.

The next time I just added a hole for the wristpin, and extended the skirt a little, No dimensioned geometry changed significantly yet when I refreshed the drawing all of the dimensions lost their association. Fortunately this time I was able to reassociate most of the dimensions except those mentioned above.

You say be more specific. If something does something all the time it doesn't seem like more specifics should be necessary. If my dimensions loose association more often than not then it seems like it should be pretty obvious.
Unless F360 just hates me or something.

[keqingsong]

Hey @yoshimitsuspeed I tried to reproduce your issue but can't seem to do it. 

Here are the steps I did: 

1. I have a saved design > created a drawing from design. 
2. Set the base view, gave it a couple of project views, and then placed a few dimensions on a hole. 
   Saved the drawing. 
3. Went back to the 3D design, rolled back to a specific instance in the timeline, changed the size of a hole, then saved the design as a new version. 
4. Went back to the drawings tab, saw the notification that the drawing was out-of-date, click "get all latest", and saw the dimension error with the hole no longer there. 
5. Went back to the 3D design, rolled all the way to the right in the timeline, saved it again as a new version. 
6. Went back to the drawings tab, saw the notification that the drawing was again out-of-date, clicked "get all latest", and the hole was back with the new dimension reflected. 

Also, what exactly did you mean when you said "So I roll back, put the model back to where it should be in the timeline"? It'd really help all of us if you can share a screencast of what you're seeing. 

[TTechN]

Hello,

loosing the associations is also a problem for us.

Trying to reproduce it with simple parts was not possible - so here it seems to work.

But doing it our normal way:

1) assembly with several linked parts

2) each part has one or several drawings

3) open from assembly, change and close a part

4) open the drawing - most the time / most of the dimension refferences are lost.

This was easy to reproduce with a two part assembly.

br

Thilo

[macmanpb]

Here too. Often the dimension reference are lost and the hole drawing module is lagging. But what i not understand, i have a MAC mid 2009 with  512MB GFX 16Gig Memory Core i7 and it is not possible to draw smooth and without lagging. Quit often my crosshair cursor within drawing is lost and flickering. 

Modeling and Scultping is fast and have a good performance, why drawing has not, what is the reason for the slow performance?

[keqingsong]

@macmanpb @TTechN Just to make sure, you guys are all saving the changes before you switch over to the drawing correct? And that's when you see the dimensions missing? 

@macmanpb I hear ya on the whole lag issue. It is not specific to your machine, and is fundamentally tied to how 2D drawings has been implemented. As mentioned in other threads, the whole 2D drawings functionality is based on AutoCAD, which was primarily written for Windows. SInce Fusion is multi-platform from the gound up, the team has to take Windows code and translate to Mac code for it to work well in Fusion. the cursor lag is one of the side-effects of this work. We've been battling this lag issue for a long time, and continuously strive to make the experience more fluid. 

[yoshimitsuspeed]

And yet AD still always gets irritated when I say that in the 21st century it's silly to make platform dependent software.
If only somone had thought to make F360 truly multi platform from the beginning.

[krithika.sundararajan]

Hi TTechN, macmanpb, yoshimitsuspeed,

Sorry to learn that you are having problems with associativity of dimensions in Drawings. We learnt about an issue where dimensions in the drawing view will lose associativy if a body's sketch contours are recreated (delete a portion of the sketch, complete it again). Are you doing something similar? If you could share more information on the steps (a screencast would be great), it would be helpful for us in digging deeper.

Thanks,

Krithika

[O.Tan]

[QUOTE]@keqingsong the whole 2D drawings functionality is based on AutoCAD, which was primarily written for Windows[/QUOTE]

I thought this isn't an issue anymore as there's already AutoCAD for Mac, which has been around for awhile?

[keqingsong]

@O.Tan Yes AutoCAD is indeed available on Mac, but it's built with different architecture and is not easily transplantable. We'll continue to iron out the experience, 2D drawings can only get better from here. 

[Anonymous]

Hi @keqingsong

Just a few specific examples are:

1. Changing a body into a component makes the drawing lose all associativity. Even if the body is within a component, changing the body to a component makes the drawing lose associations.

2. Also, if you split the body it loses association (even if the split can't be seen on the drawing.)

3. Using presspull on a face does not lose association, but using extrude does.

I can reproduce these like this  -

- Create a primitive or extrude a sketch

- Create drawing

- Go back and choose to create body into component

- Update drawing - all dimensions unlink

OR

- Create new component

- Create body in that component

- Create and dimension drawing

- Go back and create body into component (I do this a lot as I find I need certain components need sub-components not bodies)

- Update drawing - All dimensions unlink

______________________________________

- Create body (let's say a 3"W x 3"L x 5"D box)

- Create drawing so you see 3"W x 3"L face (5" can't be dimensioned, it's the depth)

- Go back and split into two (2)  3" x 3" x 2.5 boxes

- Update drawing - now, the dimensions are lost even though the depth (not dimensioned) was the only change.

______________________________________

- Create body

- Create and dimension drawing

- Go back to body and use press pull on any face

- Update drawing - Everything is okay! Cool!

- Go back, undo press pull and use extrude (join) instead

- Update drawing - Wahhh! It lost association!

---I mention this simply because it is inconsistant - Why does press pull manage to let it keep dimensions but not extrude (join)? It seems they shoud act the same, at least to me.

If you need it, I can create a screencast showing these examples tommorrow.  These are the biggest things I tend to run into.

[keqingsong]

Thanks for these examples @Anonymous - very helpful. I've shared this with our development team and have confirmed that these are workflows that we know can cause loss of associativity in the drawing. Dimensions to an object are associated to an object ID, and as a body is converted to a component or is split, dimensions associated to the body gets a new ID and become disassociated. We've tested this in AutoCAD and it showed the same behavior. With that said, we definitely think there are opportunities for us to provide a better and more connected workflow, and is something that our design teams would love connect with you more on so we can really nail down the experience. 

[Anonymous]

Sorry for the super long response!!

"dimensions associated to the body gets a new ID and become disassociated" @keqingsong

That's good to know. It gives me a much better idea of why it loses associations or how I can expect associations to be lost.

To be honest, as an end user, I'm confused as to how the dimensions are associated - so when they lose associativity I'm never sure why they were lost, especially in cases where there was no change to the actual size or shape of the part. Your explination gives me a better idea of when they will get lost, and why certain operations may change the body so that the dimensions are no longer linked.

Another reason why it may be so confusing, is that the dimension may still be visually "sitting" on the line you want it to measure, so users may think, "Why is it dissociated? It's still on the line I want to measure!" without realizing the endpoint (for lack of a better word) of the dimension is now sitting on "empty space" as it were, that it doesn't "auto-heal" to the nearest dimension-able point.

As users who may not understand exactly how programs work use the drawing suite, I can easily see someone think that adding dimensions on the drawing is just like attaching them to certain "points" on the part itself - that creating a part into a component or splitting it doesn't move or remove the points, so why do dimensions dissassociate? But in reality, you are just adding dimensions to a representation of the part, and the representation needs to be rebuilt when certain things happen.

If a user creates a drawing from a part, and then goes back to the model and does someting that would case the dimensions to loose association, would it be possible to flash a warning? "This operation caused the drawing "DWG #" to lose associativity" with the option to Continue/Cancel? I'm not saying implement this week, just asking if it is possible. I'll add it to the IdeaStation if so.

I come from a program that implemented this in a certain way (but very inconsistant) - if the dimension lost association, it could:

   1) attempt to "heal" (reassociate to the closest point, very sketchy in complicated drawings but worked okay),

   2) remove the dimension entirely

   3) Keep the dimension hanging in space (No point close enough to reassociate to).

They have a CRAZY different drawing package that I wouldn't wish on my worst enemy, though. I don't know how your dimension association code is written - is it possible to add an "auto-heal dimensions" button that would attempt to reassociate dimensions to the closest point on a drawing? This would be greately helpful in many cases - reasociating dimensions is very tedius, and (at least in my experience) most of the time, the dimensions are sitting on top of the point I want them associated to. Perhaps something else for the IdeaStation?

One question though - what is it about the press pull versus the extrude that causes the dimesions to dissassociate when extrude (join) operations are done, but not press pull, when the outcome is the same (extending a face)? As it is now, if I need to change the depth of a cavity, I don't dare go back and edit the extrude for fear of losing associativity, but I will gladly add a press pull operation to get the same result, with no impact on the drawing! In my head they are the same operation, but it is obvous they aren't treated the same in many cases otherwise they wouldn't be two seperate tools.

Well, I'm going to stop typing now Sorry again!

[scott.price]

Hey @Anonymous,

Appreciate your thoughts and ideas - the way disassociated dimensions work is definitely something we want to improve - but we're currently focused predominantly on bringing missing drawing functionality to the product. Still, you raise many good points - and I'll start looking into opportunities to improve the workflow.

As to your question, I'll need to dig into it a little bit more, but it is very odd and we might never have caught it if it wasn't for your post, so thank you for bringing it up. My best guess would be that the operations are changing the data in subtley different ways that don't impact the model in the design workspace - but are impacting how the drawings workspace updates it's references. Thanks again. And please keep bringing up any ideas or issues you come across.

Thanks,

Scott

[O.Tan]

I'm not sure if this will help but SolidEdge seems to have a wonderful way at tracking part dimension changes and does a quite good job at recovering broken dimensions.

From my observation using it, it seems that SE will try to match the referenced part to the views created in the drawing. Depending on how big the changes are, if it's hole shifts or a surface has been deleted and then redrawn to similar shape, most of the time it'll be able to reattach the broken dimensions.

Doing this method allows the user to do operations like these:

1. 1 part with 1 drawing, the part and drawing is copied and then renamed. 

2. The new drawing reference is then changed to the new part and then any changes made to the new part will allow the drawing to be updated.

Another scenario and this is where it gets impressive is:

1. Part A with Drawing A, the drawing is copied and then renamed (Drawing A Copied).

2. A new part (Part B) is created and it that has similar shape to Part A.

3. Drawing A Copied reference is then changed from Part A to Part B

4. Because the part is of similar shape, SolidEdge is able to re-associate the dimensions eventhough Part B isn't a copy or derived from Part A.

I'm open to discuss more about it, so let me know.

Regards

Omar Tan

[scott.price]

Appreciate the note, Omar -

It sounds like a very powerful way to look at associativity - but it will likely be a while before we're able to look at improvements in this area of this scope. But thanks for calling it to our attention. I'll talk to the team about it and get back in touch with any questions.

Best,

Scott

[O.Tan]

No problem, helping out in ways I can to make Fusion my preferred CAD solution 😄

[graham3848S]

So its been three years and I am still experiencing this, on top of this there still isn't any good way to dimension the holes/threaded holes that you can so easily model (meaning the information for quick easy and dynamic dimensioning is there). also there is no chamfer dimension, much like the holes I can use a note to get what I need, but then if I change the model, I have to go change all the associated notes, this is terrible. Autodesk seems to be pushing fusion pretty hard for manufacturing, and you have my employer pretty sold, but I need a tool that lets me create drawings without constantly fighting me, no program is going to be perfect, and I am quite happy with a lot of what the modeling side has to offer, but this drawing package feels more like an MS paint compared to photoshop, yeah you can still get things done, tis just slower and worse than could be done elsewhere.